animate joints

[Anonymous]

Hi,

I can't animate sub assemblies.

For instance, "conjunto elevaçao pneumatico" don't animate. Why?

joint conflits? but where?

thanks,

joao

public link : https://a360.co/3Ayv8PB

[jhackney1972 · Accepted solution]

Your Externally linked model contains around 320 files.  Since it is so many files, it will be difficult to have someone upload it to their cloud storage to work with it.

[WHolzwarth · Accepted solution]

Additionally to John's answer, I'm always having major problems with browser entries in Fusion 360.

For comparison, I've exported the fileset to STEP and opened it in Inventor. The resulting browser seems to be a good start for an Inventor Studio animation, after applying new constraints or joints.

[WHolzwarth]

Meanwhile I've played with the centering mechanism for the feeding device in Inventor Studio. See Screencast.

https://screencast.autodesk.com/Embed/Timeline/49fb831a-abeb-4002-a880-dd13906ab180

Perhaps someone can show similar in F360

[TrippyLighting]

@WHolzwarth I believe the only way you can do that in Fusion 360 is with a motion study.

The animation workspace in Fusion 360 does not honor any of the joints and as such IMHO is useless for such things 

[WHolzwarth]

Thanks for your opinion, Peter.

I didn't try much with F360 motion studies, but I think, doing this motion needs a lot of knowledge.
Inventor Studio sometimes is tricky, too. But more can be done there.

[Anonymous]

Hi John,

so when we have a model with a lot of files (like mine) the Fusion 360 has problems.

The best way is opening the model in another program  (like Inventor).

There is a better strategy to do the big models in Fusion 360? (if I use less files, it will be more complicated to do the entire model).

Thanks,

Joao

[WHolzwarth]

Entire model will be a challenge in Inventor Studio, too.

I'm just doing another animation for the back clamping of the workpiece. Perhaps later in the evening or the next days.

[Anonymous]

Hi Peter,

take in account your experience, how do you see the model that I made? To many files? I tried to do small model units and then aggregate all in one big model, it's correct or I need to change my approach?

Thanks,

Joao

[TrippyLighting]

Generally, breaking down a large assembly into smaller assemblies is what I recommend and also practice. Because I like to develop parts in context and like Fusion 360's top down design abilities I don't create everything as a separate file, but that is personal preference, not necessarily "best practice".

I only got around to load down your design this morning and  have not had the time to go through it in detail.

It is indeed a very "clean" design with no warnings or errors in the timeline, and everything seems to be properly joined.

Can you describe in more detail what problems you encountered in this design ? Are those performance problems, e.g. in creating joints, or moving assemblies etc. ?

Your design has over 2000 components with more than 8000 bodies. I am assuming that most of the multibody components consist of many hundreds of surface bodies. Is that correct ?

[WHolzwarth · Accepted solution]

Looking at the STEP file out of F360, imported to Inventor, I found no surface data in the components.

But there are lots of duplicate files for cable chain components, ball bearings and linear roller parts.

Attached is the link for another screencast for the clamping device at the end of the machine. Best view is 2x speed, but it begins to be a problem here for my system.

https://autode.sk/3TcP5D7

[TrippyLighting · Accepted solution]

What caught my attention is the mixture of faces with a regular material color mixed with faces with the brownish color in what appears to be a single body. That brownish color indicates that the surface normal is  pointing in the wrong direction. Surely enough, that "part" consists of hundreds of unstitched surface bodies.

I believe these surface bodies cause "some" performance problems, for example they are responsible for the slow .f3z upload of the design and also the relatively slow (but not bad) loading of the design.

I've previously shared some of my designs with performance problems with the Fusion 360 team and have been asked whether I would be interested in working with them on performance improvements.
This would be a great design to test things out.

@Anonymous would you be OK with me sharing this design with the Fusion 360 team ?  

[TrippyLighting]

---

@WHolzwarth wrote:

Looking at the STEP file out of F360, imported to Inventor, I found no surface data in the components.

But there are lots of duplicate files for cable chain components, ball bearings and linear roller parts.

---

In Fusion 360 those aren't individual files, but they are all duplicate components with their own unique bodies. They should ideally component instances.

That is indeed going to eat a lot of memory!

[TrippyLighting]

Here's another thing.

This entire chuck assembly is imported geometry. There is no good reason to turn on the timeline. This only increases file size by at least factor 2 and provides no benefit as no parametric changes are made.

Nothing moves as everything is assembled with one rigid group.

[Anonymous]

Problem: when I try to make any move with sub-assemblies  in the main model, they don´t move. I reckon that the model is to big and heavy.

I like to "break" the main model in many multibody components just to control more easy my designs. I don't know if it is the better strategy.

[Anonymous]

Many thanks, I will look and implement your solution

[Anonymous]

This assembly cames from solidworks and I really don´t need the timeline

[Anonymous]

Yes, you can share with the Fusion 360 team